Element Membrane M3D6
Moderator: bernd
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
Element Membrane M3D6
Hi,
I would like to simulate a spherical shell with internal pressure, like a ball, with hyperelastic material (Neo Hooke and Yeoh), to compare with analytical solution.
But the model never converges, always for same reason :
"*ERROR : too many cutbacks
best solution and residuals are in the frd file"
I test some solver and different increment (direct, iteratif, cholesky, explicit, in INP writing).
1) Do you know if calculix can solve spherical shell problem?
2) How can I change cutbacks?
3) Which solver is it better?
May be it will be better to ask this question at Guido Dhondt, because it is a calculix problem...
I would like to simulate a spherical shell with internal pressure, like a ball, with hyperelastic material (Neo Hooke and Yeoh), to compare with analytical solution.
But the model never converges, always for same reason :
"*ERROR : too many cutbacks
best solution and residuals are in the frd file"
I test some solver and different increment (direct, iteratif, cholesky, explicit, in INP writing).
1) Do you know if calculix can solve spherical shell problem?
2) How can I change cutbacks?
3) Which solver is it better?
May be it will be better to ask this question at Guido Dhondt, because it is a calculix problem...
Last edited by Groguigui on Fri Apr 21, 2017 8:35 am, edited 1 time in total.
Re: ERROR : too many cutbacks
Hi,
I suspect you face a problem of material instability (well known for elasto-plasticmaterials).
- Please try first with an elastic material --> it should cpnvergence with the static solver
- then for a elasto-plastic material (for example sigma=KEps^n). I do not exactly remember the formula but if n=0.18, you should get the instability when EpsBar (equivalent plastic strain) is around 0.12.
To solve this, best solver is dynamic, implicit. You need inertia to stabilize the solution.
Try something like,
*Dynamic
0.01,1.,1e-7,0.01
BR
I suspect you face a problem of material instability (well known for elasto-plasticmaterials).
- Please try first with an elastic material --> it should cpnvergence with the static solver
- then for a elasto-plastic material (for example sigma=KEps^n). I do not exactly remember the formula but if n=0.18, you should get the instability when EpsBar (equivalent plastic strain) is around 0.12.
To solve this, best solver is dynamic, implicit. You need inertia to stabilize the solution.
Try something like,
*Dynamic
0.01,1.,1e-7,0.01
BR
Last edited by sodelo on Fri Apr 07, 2017 7:52 am, edited 1 time in total.
Re: ERROR : too many cutbacks
Activate user defined incrementation , the defaults tend to not be sufficient when dealing with non-linear problems.
Then set the control parameters manually
Then set the control parameters manually
Re: ERROR : too many cutbacks
Thanks,
Finally, I found how solve my problem : I used *Controls fonction to set increments and cutbacks.
http://web.mit.edu/calculix_v2.7/Calcul ... de179.html
Finally, I found how solve my problem : I used *Controls fonction to set increments and cutbacks.
http://web.mit.edu/calculix_v2.7/Calcul ... de179.html
Re: ERROR : too many cutbacks
you can set them in FreeCAD CalculiX solver object too. Means no need to edit the input file.Groguigui wrote:I used *Controls fonction to set increments and cutbacks.
Re: ERROR : too many cutbacks
Yes Bernd, I saw, but I think isn't possible to set cutback in FreeCAD. Anyway, actually I have another problem.
Do you know why FreeCAD solve a stress in third dimension when we use a shell element? Usually, it must be zero with plane stress hypothesis.
Actually I would like to solve a hyperelastic spherical problem under pressure. But I don't understand why results are different to analytic solution.
Do you know why FreeCAD solve a stress in third dimension when we use a shell element? Usually, it must be zero with plane stress hypothesis.
Actually I would like to solve a hyperelastic spherical problem under pressure. But I don't understand why results are different to analytic solution.
Re: ERROR : too many cutbacks
Results in local coordinate system are new for shell elements in ccx 2.12 * ccx 2.12 creates automatically local coordinate system for shell elements, but projecting of global x-axis could be strange for elements with normal direction close to x-direction.
Older versions print stresses in a global c.s.! * results are by default in the global c.s. The local coordinate system must be triggered in the .inp file by
Plane stress (or plane strain) needs special element types which can be used only on 2D model in xy plane in Calculix. So I would expect nonzero normal stresses on your shell elements.
*EDITED
from http://www.dhondt.de/new_calc.htmFor shells a local coordinate system is automatically established by projecting the global or local (if defined by the user) x-axis on the shell surface.
Older versions print stresses in a global c.s.! * results are by default in the global c.s. The local coordinate system must be triggered in the .inp file by
Code: Select all
*EL FILE, global=no
S, E
*EDITED
Last edited by fandaL on Wed Apr 19, 2017 2:40 pm, edited 1 time in total.
Re: ERROR : too many cutbacks
And you're right!So I would expect non zero normal stresses on your shell elements.
I understand, that is why I have non zero normal stresses, because applied pressure is normal on my shell elements. In fact I didn't work with plane stress hypothesis.Plane stress (or plane strain) needs special element types which can be used only on 2D model in xy plane in Calculix.
1) How can I find this elements types? Does it exist actually in FreeCAD? In calculix?
2) What calculix version is in FreeCAD 0.17? I don't know where is this information.
3) Sorry I have already ask this question, but I forgot the answer, it is possible to solve a problem with shell AND volumic mesh with calculix and/or freeCAD? Like a volumic cube with different materials on each faces and inside.
Re: ERROR : too many cutbacks
You can look to the manual http://www.feacluster.com/CalculiX/ccx_2.11/doc/ccx/ under Theory/Element Types there are several plane stress elements. After writing .inp file in FreeCAD you can search in the file line like1) How can I find this elements types? Does it exist actually in FreeCAD? In calculix?
Code: Select all
*Element, TYPE=S6, ELSET=Eall
However, it will most probably fail on spherical model. You can define plane stress elements only in xy plane.
2.8p or 2.11 You can find it, when you click “Run Calculix”, in the beginning of the printed log2) What calculix version is in FreeCAD 0.17? I don't know where is this information.
Discussion about 2.12 https://forum.freecadweb.org/viewtopic.php?f=18&t=21680
It should be possible in CalculiX. FreeCAD does not yet support meshes combining 2D and 3D elements.3) Sorry I have already ask this question, but I forgot the answer, it is possible to solve a problem with shell AND volumic mesh with calculix and/or freeCAD? Like a volumic cube with different materials on each faces and inside.
Re: ERROR : too many cutbacks
Hello,
Freecad bundles pretty outdated ccx.exe. So better upgrade to ccx2.12.
If you have a 3d-shape like a balloon, and you have to avoid bending stress. then membrane elements are first choose.
See http://www.dhondt.de/ccx_2.12.pdf
Page 92 cit:
External forces (and pressure loads) are applied normal to membrane's face
Internal forces are aligned tangentialy to membrane's face and leads to plain deformation.
Curvature is only done on element's edges.
Freecad bundles pretty outdated ccx.exe. So better upgrade to ccx2.12.
If you have a 3d-shape like a balloon, and you have to avoid bending stress. then membrane elements are first choose.
See http://www.dhondt.de/ccx_2.12.pdf
Page 92 cit:
Membrane elements could not bend. They stay plain in space.6.2.14 Three-node membrane element (M3D3)
This element is similar to the S3 shell element except that it cannot sustain
bending. This is obtained by modelling hinges in each of the nodes of the
element. Apart from that, all what is said about the S3 element also applies
here.
External forces (and pressure loads) are applied normal to membrane's face
Internal forces are aligned tangentialy to membrane's face and leads to plain deformation.
Curvature is only done on element's edges.